This topic explains how to create a metric (module) helical gear in pro engineer / Creo using relations and formulas. Helical gears are widely used gear types after spur gears. The nomenclature of spur and helical gears are all same except for the helix angle and its relevant parameters.
In spur gears the gear teeth is straight and parallel to the axis of rotation but in helical gears the gear teeth is at an angle to the axis of rotation and follows a helical path (aka Helicoid) along the pitch circle diameter.
The angle between the axis of rotation and the tangent line through the helicoid is called the helix angle. First lets go through the input parameters, relations and formulas of helical gear.
Typical input parameters for helical gears are given below. I have taken some example values for this topic. (All values are in “mm”).
The formulas given below are used get the necessary parameters to model the gear. You can abbreviate the terms if you want.
The input parameters needs to be created using Tools → Parameters. If you have a gear data table, you can use them directly instead of going through the formulas.
Formulas for helical gear:
Transverse_module = normal_module / cos (helix_angle)
Normal_circular_pitch = pi * normal_module
Transverse_circular_pitch = pi * transverse_module
Transverse_pressure_angle = atan ((tan (normal_pressure_angle))/(cos (helix_angle)))
Outer_Diameter = pitch_diameter + (2 * normal_module)
Root_diameter = pitch_diameter – (2 * 1.25 * normal_module)
Base_diameter = pitch_diameter * cos (transverse_pressure_angle)
Normal_tooth_thickness = (pi * normal_module) / 2
Transverse_tooth_thickness = (pi * transverse_module) / 2
Lead = pi * Pitch_diameter / tan (Helix_angle)
Formulas for Diametral pitach (DP) standard is here.
Although I use WF 5.0 to explain most of the steps here, the method is same for any version of Creo or Pro engineer.
You just need to locate the commands.
1. Make an extrude for the gear blank. Don’t bother about the dimensions. Just give any value for now.
2. Go to Tools → Parameters from the main menu. Create the input parameters and the enter the values as shown in the image below using the add button.
3. Go to Tools → Relations from the main menu and enter the relations. Copy paste the gear formulas given above.
4. Create three circles for Outer dia, base dia and pitch dia using sketch and name them as shown below in the model tree. Give any dimension for now.
5. Now we have to relate the formulas(dimensions) to the respective sketches. To do that, see the video below. You need to regenerate to see the result. Relate the dimensions to the respective sketches (i.e Pitch_diameter parameter for Pitch_dia feature)
Note: If you open the parameters windows now, you will see some additional parameters. This is because we created new parameters through formulas/ relations.
6. Create a new coordinate system at the center of the gear blank using the datums and front face as shown in the image. Name it “GEAR_CSYS” for reference purpose. Make sure that the Z direction points outside, X horizontally and Y vertically. I recommend to create it as shown in the image (X and Y in positive direction). This coordinate will be used to create the involute curve from equation.
7. Now the involute curve has to be created. In ProE wildfire versions, go to Insert → Model datum → Curve or use the short cut button. This will open up the curve menu manager. Click on From equation and Done. Now you have to select the newly created “GEAR_CSYS” coordinate. Then select “Cartesian”. This will open the text window.
To open this in Creo, type Curve in the search box at the top right corner and select “Curve from equation” from the list.
Now paste this equation in the text window.
Base_radius = Base_diameter / 2
Angle = t*90
Cir_len = (PI * Base_radius * t ) / 2
X_PNT = Base_radius * cos(Angle)
Y_PNT = Base_radius * sin(Angle)
x = X_PNT + ( Cir_len * sin(Angle))
y = Y_PNT – ( Cir_len * cos(Angle))
z = 0
Save the text window and close. Click done. This will create the involute curve.
8. Create a sketch for Transverse_tooth_thickness (this is circular tooth thickness in case of spur gear) at pitch diameter from the intersection point of involute curve and Pitch diameter as shown in the video and relate the dimensions to the parameter.
9. Now, Create a new point at the center of the transverse_tooth thickness curve using point option. To do that, go to Insert → Model datum → Point → point. Now click the newly created curve and enter 0.5 in the input area as shown in the image.
10. Create a new datum using the point created in step 9 and the center axis of the gear as shown in the image. This will be used to mirror the involute curve.
11. Mirror the involute curve using the datum created in step 10. The model will look like this.
12. The helical path (helicoid) has to be created now through which the teeth section will sweep. To do that, go to Insert → Helical sweep → Surface in wildfire versions and in Creo select Helical sweep under Model tab and then click Surface icon in the feature dash board. See below images.
13. Accept the options “constant, Thru axis and right handed”. Select the datum created in step 10 as the sketching plane for this. Select the orientation you want and go into sketcher.
For sweep profile, draw a line from the start face to the end face using references. Make sure that the start point is from the face where you modeled the transverse section. Draw the center line. Create a diameter dimension as shown in the above image and enter Pitch_Diameter. This will relate the dimension to the pitch diameter parameter. When done, click ok and come out of the sketcher.
When asked for pitch, type “Lead” in the input area. This will relate the dimension to the Lead parameter
Next, to define the section, draw a line from the section center to the center line of the gear as shown bellow.
Complete the helical sweep feature and when done the model will look like the image shown below.